Rotate part AND sketch.

I created an assembly and noticed a part was oriented incorrectly. I rotated the part 180 to its proper orientation but when I went to edit the sketch to make small adjustments I noticed the sketch had remained in its original (now incorrect, off by 180) orientation. Must be simple but how can I rotate both the part and the sketch? Or just the sketch and have the extrusion follow?

Hi @larry_hawes, great way to post a question, and welcome to the forum BTW. One thing we always suggest is that if your doc isn't confidential post a link to it and we can actually demo our suggestions to you.

What you're seeing is normal, and as ever with CAD there are may different ways to approach this. Please excuse me if I'm telling you things you already know.

(1) OS works down the feature list each time you open the doc or rebuild any feature, it's "just" a list of commands run in order. So as you've seen the order matters to a degree. Have you used the "roll back bar" yet? If you go back and edit the sketch you'll see this happens before the rotate. As such there is no need to rotate the sketch as well.

(2) You can as you point out if you rotate the entities in the sketch and then you don't need to rotate the part. There is a "sketch transform" tool with a manipulator triad that will allow you to move and / or rotate stuff. (Note you can drag the circle at the origin of the rotate triad to define where you want to rotate things about.) Details in the help here:-https://cad.onshape.com/help/index.htm#cshid=sketch_tools_transform

(3) There's no real need to have things in the part studio in the orientation that you need them in an assembly. Think of modelling a bolt. You might model that once, and use it over and over again in multiple orientations. Have a look at "mate connectors", they're available in assemblies and partstudios and once you've got the hang of them things are so much easier.

(4) Slightly on topic. OS excels in multi-part-modelling. By which I mean modelling parts that fit together in one partstudio. By doing so you can have one part drive the dimensions and orientation of others. Change one dimension and all the others rebuild around it.

Hopefully some of that helps. Feel free to shout if you need it, lots of helpful folks here.

Oh and I would really recommend signing up for one of Cody's "Introduction to Onshape" webinars. They're free, and a great way to pick up the essentials of the software.

THANK YOU OWEN, Lots to digest for a new user but will explore and see if I understand the concepts. LOVE the idea of modeling multiple parts in one part studio but don't quite understand that dynamic yet. Seems like it would solve a lot of problem with multiple parts in multiple studios and fitting them perfectly in an assembly later. LOTS to learn and your help is greatly appreciated.

I hope the video below describes the problem and I am sure there are reason to not have to perform the operation as described but if one were to try and rotate a part and all of its sketches how would/could that be accomplished?

Hi @larry_hawes as Owen says the transform tool cannot move sketches (or any other features before it). It is only used to move solid bodies. When you edit the sketch it reverts back to the time when it was created.

Don't confuse a part Studio with an assembly. Onshape does not care in which orientation a part is modelled because you can fix it in an assembly.

I think I finally understand the paradigm and was able to simply rotate the part in the assembly using the Triad Manipulator. Not sure why I missed that so many times but sometimes I'm not the sharpest tool in the shed.

Hello! I've a question that seems to stump me on many types of CAD software. I'm used to modeling in Rhino and I remember Autocad being able to do this easily but I can't seem to find a way to do this in a single part on OnShape.

So here's what I'm trying to model -

More accurately, the outer shell of it (I'm trying to do a 3D print of the negative of the shell). Now the main body is relatively simple, except for the "nose", or the speaker head.

I've done a basic side profile sketch with a revolve so that gives me the main body shape (fillets etc will come later), but what I need to do now is create an extruded ellipse, rotate that, then sweep/loft the nose and main body together.

Thing is, I can't seem to find a way to rotate it along the Z axis, and I'm pretty sure I'm missing something. Logically it doesn't make sense to do this in Assembly because they're the same part and will get booleened later with the sweep.

I'd also need to make a loft/sweep after to join the two parts, which will also be on an angle, and I'm really not sure how to manipulate sketches (especially an angled nose) in two planes to be able to do that. Any clues please, anyone?

Hi and welcome. Always easier to help if you post a link to your document, that way we can take a copy and demo our suggestions.

So a couple of things here.

(1) You could do as you describe and move it into place. You'd need the "transform" function to do so. There are many transform options, the transform by mate connector is highly recommended, as is the rotate.

(2) Instead of all that much better to model it in the final position in the first place. I'd start with looking into the "plane" function. Once you have some planes in the correct places you'll have a far cleaner model and it'll be easier to understand the design intent.

Yours is more about surfacing and it'd be nice to collect these into a surfacing area in this forum.

Like Owen says, there's a lot of people here that'll help you.

I'd use a loft to make a connection between your parts. You will have problems because you'll have issues with the loft folding on itself and failing. To prevent this, you'll need to add guide curves defining how the loft transitions from one section to another. The easiest way to define a guide curve is to create 3D fit spline and define in detail how the loft behaves.

Positioning of the parts is basically compound sketches which will produce any vector anywhere in space. I believe with 2 sketches you can define 3 translations & 3 rotations in a controllable fashion. I'd put a mate connector at the end of the vector and then use transform with mate connectors. Transform with mate connectors is the only transformation that allows control of all 6 degrees of freedom in one transform. Individual transforms would require 3 rotate transforms and then a 1 translation transform. This is why I'd use the compound sketch method, mate connector & 1 transform using mate connectors.

Also with these curves, you be able to define the shape required for a good looking product.

The setup before transform with mate connector, using compound sketches:

I believe you can position anything anywhere using this design pattern: